Easiest way to get a flat on the inside of a hub

We don't machine metal parts for our customers, those parts are always farmed out and we do the end assembly. Got a new preliminary design from a customer and their "hub" is fairly standard (has an ID, OD, a flange with boss, set screw) but the ID has a flat in it . My machining knowledge tells me this will be rather difficult to achieve. Volumes are low so any investment casting, even if accurate enough, is out of the question (as is laser cutting the ID). Outside of broaching (which would require a customer broach), is there any other means of getting a flat on the inside? Material is stainless 316 and the nominal ID is 48 MM and the flat is at a radius in the center of the flat at 23 MM. The hub bore is 8.5 MM thick.

My only though is to machine out the bore but I'm not even experienced enough to know what tools to use to carve out the inside of the hub or if this could be done on a CNC lathe with live tooling. I guess that's why I'm asking here!

Update: here's a simple diagram of what they want:



Thanks,
The Dude

I don't follow your description all that well TBH, but if I understand what you mean correctly then:

If quantity is low, wire edm first and then bore. If the geometry allows it, you can do both bores in one setup with a back boring bar, if not it'll have to be bored from either side.

Your customer may want to consider a redesign depending on the quantities as it will be an expensive process no matter how you go about it.

gregormarwick said:

I don't follow your description all that well...

Click to expand...

Thanks, it is tough to take works and assemble a mental picture. I updated the post with a simple diagram that hopefully illustrates it better.

The Dude

Customer has specified a really expensive part, at least in small quantities. Advise them to redesign for a more cost-effective production technique.

If they insist on the flat, ask if they will accept 1) clearance runouts into the body of the part at each end of the flat for a small endmill, or 2) a circular chord key pinned, welded, or glued into a circular bore, or 3) pay for the NRE to develop a casting pattern/mold.

Probably has the same (or worse) cost issue as casting or laser cutting, but you might see if someone can sinter the blanks for you.

They're doing it wrong, go buy a QD bushing hub and design whatever mating part to use the QD bushing.

If needed to be to the print exactly - Wire EDM

If some clearance rads in the corners is allowed, then you could mill it in.



------------------------------

Think Snow Eh!
Ox

sfriedberg said:

clearance runouts into the body of the part at each end of the flat for a small endmill

Click to expand...

In case you don't get the visual. They can be made much more subtle than this:

Thanks guys, you have for the most part confirmed my suspicions. I just wanted to be certain that I hadn't overlooked anything. I did think about EDM and immediately threw it out as too expensive.

The Dude

It would be possible to mill it without the clearance offered above, but rather with rounded corners at the transition to flat... and then do minimal broaching of just those corners. The broach(es) would be half-radiused, half-straight, but since you're profiling the outside of the broach, it's easier and hopefully cheaper. Broach would ride on a "carrier" for guidance. (I'm sure there's a more accurate term of art than that...) Or, the right size/shape of shaper bit could handle it.

Re-design is better than my suggestions, though.

Chip

The Dude said:

I did think about EDM and immediately threw it out as too expensive.

The Dude

Click to expand...

I get that all too often.
Some joker designs a $20 part but "needs" it for $10.

I'm happy to make a $10 part, but you need to take the other $10 out of the design / tol / finish / material / qty requirements.

I may be able to help redesign the part to meet your app/cost factor ratio, but I can't just make it cheaper just because you "need to be in this target range".


-------------------------

Think Snow Eh!
Ox

sfriedberg said:

Customer has specified a really expensive part, at least in small quantities. Advise them to redesign for a more cost-effective production technique.

If they insist on the flat, ask if they will accept 1) clearance runouts into the body of the part at each end of the flat for a small endmill, or 2) a circular chord key pinned, welded, or glued into a circular bore, or 3) pay for the NRE to develop a casting pattern/mold.

Probably has the same (or worse) cost issue as casting or laser cutting, but you might see if someone can sinter the blanks for you.

Click to expand...

Indeed, suggesting the customer one of those alternatives is the best start. Often the design just reflects an ignorance of the fabrication process.
If the current design cannot be changed, one way is to mill the part with radii on the flat/bore transition and then to remove the radii in a shaper using correctly formed tool